What's new
What's new

Bad chatter marks when profiling tight corners

stephon0913

Plastic
Joined
Aug 12, 2011
Location
Portland, OR
looking for some advice when profiling tight (sometimes close to a vertical wall) corners on patterns. these are made from a red urethane called tooling board. Its fairly hard stuff. the issue is that some of the corners have to be filleted pretty tight (up to 1/16 fillet) that mean getting into tight corners with a 1/8" ball endmill sometimes having to hang my tool out up to 3 inchs. I work in the pattern industry similar to mold making, however molds usually have enough draft along the walls to not have to worry about this. because of the tool length i need, any chatter i get while cutting rides up the side of the wall and looks horrible. ive attatched some pic showing what im talking about. because of the almost vertical walls i cannot use a tapered tool holder. Any advice or suggestions to this issue?

thanksIMG_0898.jpgIMG_0899.jpgIMG_0897.jpg
 
Are you programming your fillet tool right up to the wall? Try leaving .001 to .002 per side on the walls so the tool won't actually touch the already machined surfaces.
 
That second picture looks like tool deflection. Is it possible to slow the rpm's down when in the areas giving you grief?

yes. It's all from tool deflection, im using a 1/4 ball endmill thats hanging out 3" from the collet. i usually run these at 12k rpm at 50 ipm about .001 chipload per tooth. I have tried slowing it with very limited success.
 
I would try a long reach stub flute ball endmill from Harvey tool and maybe even have them reduce the l.o.c. to just above the ball radius. I would imagine a tool that long and skinny might start to whip at those spindle speeds, I would cut back to maybe even 2 to 3k just to see if you can get it to cut without chatter and then work the speeds up.
 
The joys of running small tools hanging out 5 miles! My experience is you need to keep the RPM up where you're at to get as much SFM as you can, keep the feed up as well, and start reducing stepovers / depth cuts until it's happy. This is not the time to be making small changes. For example, if you're using .005" stepovers now, don't try .004". Try .001".

Once you get as much chatter out of it as you can (likely not all chatter will ever go away), then start bumping up the feedrate until it gets sad again, or the tool breaks. Now you'll be in a workable range.
 
I've had some luck with profiling just the corner with a helical ramp at a moderate step down. You actually need a toolpath in the form of a small triangle to clean up what gets left from a larger diameter tool that was used to rough the corner with.
 
I've had some luck with profiling just the corner with a helical ramp at a moderate step down. You actually need a toolpath in the form of a small triangle to clean up what gets left from a larger diameter tool that was used to rough the corner with.

its more of a 3D contour that im profiling, yes in 90 degree corners I usually take perpendicular cuts seems to help vs just using the 3D collapse method.
 
Ahhhhh, looks familiar. Things that have helped me reduce chatter, and better blend in rest finishing. Beside some good advice re stepovers/stepdowns above.

-Climb only. Yeah it takes longer, but it's worth it. 90% of the time I can get away with a combined path, but on steep sidewalls with long sickouts it always gouges on the conventional pass.
-Leave meat on. Try leaving a thou or two on when programming. It's easy to feather in the edges, but if the shank touches the side wall it will leave a mark.
-Rest rough first. Try and give the cutter the same "bite" every time, and you will get less gouges.
-Relieve the shank and just behind the tangent point of the ball a few thou.
-Set all your tools at their running temperature. Run them for a bit at the feeds and speeds they will run at then set your z offset. You will get near perfect blend lines.
-Look into getting a universal angle head, and a good efficient way to program it (rhino w/madcam). Some jobs we get would be very difficult to do without it. I also would rather use that with a 1/8" ball than to try and hang the same tool out 2-3".
-Don't try and do a 1/16" rad with a 1/8" cutter.... always use a smaller cutter so you can "drive" it around the curve.
-Break up your toolpath. With Edgecam's rest finish it will just collapse in on itself to pick out the rad. That means it will drive up and down vertical walls. I like to break those up and "profile" (z level) down the vertical walls, then rest finish the flatter areas separately. Not much more programming work, but noticeably better results.
 
Other thing to look at, what kinda HSM settings does your control give you? Whilst most high speed - look ahead controls have a few diffrent accuracy modes, some even let you set a max allowable deviation. This effectively lets the control not drive into a sharp corner, stop then accelerate out of said corner. By not pausing, the cutter remains cutting - loaded and does not chatter like it does parked in a corner once its done cutting. Trade off is you lose some accuracy, but it can be so slight as to be irrelevant, especially on stuff like that.
 
Chatter on the walls is an issue with many causes, but the corner thing is kind of easy to fix. If you pre-drill smaller, then finish drill with the end mill you're going to cut with, you can avoid the momentary overload that occurs when you suddenly up the engagement by driving the cutter into the corner.
 








 
Back
Top